Sketched Symbols in Autodesk Inventor: Follow the Leader

Editor's note: Scroll to the bottom of this article to watch the video version of this tip.
This tutorial courtesy of IMAGINiT Technologies.

I find it really irritating when sketch symbols or text that I've placed on a drawing at views and balloons will not stay where they were intended once that view or balloon is relocated. You could just select everything related to the view and drag it to its new location on the same sheet, but good luck trying to place that view onto a different sheet. The potential for error now is greatly increased, as callouts can be missed or forgotten. And those errors, of course, cost time and money. (Not to mention, I’m currently playing a timed minesweeper game and I need to get back to it ASAP.)

Follow That View

In this example, we are going to look at having a sketched symbol follow the drawing view. We will start out by having a sketched symbol that has geometry, prompted text, and the ability to extract the description of the part in the view.

When placing the sketched symbol:
1. Select the sketch symbol to place
2. Touch the object in the view
3. Fill out any prompted text
4. Click on the sketch symbol, then drag the symbol to its desired location. This will add a leader from the object to the sketch symbol. (Don’t worry, we will
get rid of that annoying leader.)
5. Double-click on the sketch symbol
a. Uncheck the “Visible” option
b. Do not uncheck the “Leader” option; this will basically undo what we are
trying to accomplish.

Now you are able to move the view around on the current sheet, as well as move the view to a different sheet with the sketch symbols following the view!

Follow that Balloon

In this example, we will look at something that will hopefully be addressed in a future release of the software as a permanent solution. When checking drawings, I’m sure we all have grabbed our coffee and highlighters and started verifying that we have all of the correct balloons and quantities called out per the parts list on the drawing. So much time is wasted verifying that all 58 flat washers were accounted for in the drawing! Having the ability to add quantities when placing balloons and keep a running tally would be amazing.

Unfortunately, this tip won’t address that specific issue, but it will help you keep quantities callouts and any other sketch symbol attached to the balloon so when adjusting the views, everything stays put. Here, the sketch symbols will just consist of just prompted text.

When placing the sketched symbol:
1. Select the sketch symbol to place
2. Touch the edge of the balloon
3. Fill out any prompted text
4. Click on the sketch symbol, then drag the symbol to its desired location.
This will add a leader from the object to the sketch symbol. (Don’t worry,
we will get rid of that annoying leader.)
5. Double-click on the sketch symbol
a. Uncheck the “Visible” option
b. Do not uncheck the “Leader” option; this will basically undo what
we are trying to accomplish.

Extra Credit

Even though I subscribe to the "one part, one drawing" workflow, it is still common for companies to have a workflow where there are multiple parts being detailed on the same drawing. The problem arises when you place the parts list. It will only show items from the view that has generated it. Here is what I do in this situation.

Let’s say you have three channels that are named as follows:
1. 100K200-1
2. 100K200-2
3. 100K200-3

Create a “dummy” assembly named 100K200-0 and place all of those channels in that assembly. This assembly does not need to be placed in the drawing in order to use it as a way of generating the parts list. Simply select the “Browse for File” option after selecting “Parts List,” select the 100K200-0 assembly, and place your parts list. This will eliminate the need to manually re-enter all of the line items — a process which lends itself to errors. Again, this will save time and money and get you back to sweeping those mines!

About the Author: Anthony Dull

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